2 of 66

Module 04 Topics

Demonstration: ANSYS Mechanical Postprocessing
Section Planes
Probe Tool
Charts
Scoping Results
Coordinate systems
Linearized Stress
Error Estimation
Convergence

Stress Singularities
Convergence and Scoping
CAD Import
Defining Parameters in Workbench
Using the Parameter Workspace
Updating CAD Parameters
Workshop 04.1: Processing Results
Workshop 04.2: Parameter Management
Appendix 04.1: Additional Postprocessing

This module covers Postprocessing, validation, CAD, and parameter management topics that are common to all mechanical analysis disciplines:

March 10, 2016

3 of 66

04.01 Demonstration: ANSYS Mechanical Postprocessing

This demonstration provides an overview of common postprocessing functionality:

Viewing Results
Legend Controls
Contour Controls
Postprocessing Utilities
Scoping Results
Exporting Results

[video file: 04-Postprocessing.mp4]

March 10, 2016

4 of 66

04.02 Section Planes

Section Planes are used to slice the model for viewing.

Select the “Draw Section Plane” icon, then click-drag with the left mouse button.
Section planes can be turned on/off using the check box in the details view.
Delete section planes using the delete icon.
Edit section planes by highlighting desired plane name and using the ‘handle’ in the Graphics window.
Can use local coordinate systems to automatically create a section plane (XY plane).

Click on one side of bar to cap view

RMB

Move a slice plane by dragging handle

March 10, 2016

5 of 66

04.03 Probe Tool

The Probe Tool:

Can be scoped to numerous entities depending on the probe type and results can be made parametric.
The orientation of the result item can be with respect to global or local coordinate systems.

March 10, 2016

6 of 66

04.04 Charts

Combine results data from multiple steps (static or transient) into charts and/or tables:

Select “New Chart and Table” icon.
From the details “Apply” the desired result(s).

Use the CTRL key to select multiple results.

Select desired display items in details.

March 10, 2016

7 of 66

04.05 Scoping Results

Some examples of scoping results on surfaces/parts:

Result scoped to a single part

Result scoped to a nodal named selection

Result scoped to selected surfaces

March 10, 2016

8 of 66

04.05 Scoping Results

We can also scope results to nodes and elements directly:

Select the Node or Element toolbar button selection filter.
Select the desired entities in the graphics window.

March 10, 2016

9 of 66

04.05 Scoping Results

Contour plots across multi-body parts are available:

When you select Averaged as the display option, setting detail Average Across Bodies to ”Yes” (the default value is ”No”) averages the results across separate bodies the model.

March 10, 2016

10 of 66

04.05 Scoping Results

For more in-depth information on this and �several other postprocessing topics, see�Appendix 04.1: Additional Postprocessing

March 10, 2016

11 of 66

04.06 Coordinate Systems

Results containing directional components can be transformed into a local coordinate system:

In result details select coordinate system from the drop down list.

Stresses in Local Cylindrical Y-Direction

March 10, 2016

12 of 66

04.07 Linearized Stress

Using the path plot feature a linearized stress calculation can be plotted (commonly used various structural codes such as ASME).

March 10, 2016

13 of 66

04.08 Error Estimation

You can insert an Error result based on stresses (structural), or heat flux (thermal) to help identify regions of high error.

These regions can indicate where the model could benefit from a more refined mesh.

Error plots are used to identify regions where large energy changes occur between adjacent elements.

The actual energy value in the legend is of little significance on its own.

Mesh Refinement

March 10, 2016

14 of 66

04.09 Convergence

In most finite-element analyses as the mesh is refined one expects to get mathematically more precise results. How much refinement is “enough” usually requires experience and engineering judgment. The Mechanical application has a convergence tool that can help assess the mesh quality.

Obtaining an optimal mesh requires:

Having criteria to determine if a mesh is adequate.
Adding more elements only where they’re needed.

Attach convergence to a result item and set the “allowable change” in the convergence details.

Specify maximum number of iterations in the Solution details.

March 10, 2016

15 of 66

04.09 Convergence

After the solution is complete one can view the results normally:

The Convergence history shows the trend for each refinement loop.
Displaying elements in the results plot shows the last mesh (the mesh branch always displays the original mesh).
Symbol next to convergence branch indicates success or failure.

Convergence

Divergence

March 10, 2016

16 of 66

04.09 Convergence

The Convergence tool cannot be used if:

The model contains mesh connection object
You have an upstream or a downstream analysis link
You import loads in the analysis

To use Convergence, you must set “Calculate Stress” to “Yes” under Output Controls in the Analysis Settings details panel.

March 10, 2016

17 of 66

04.10 Stress Singularities

In structural analysis there are several situations that can cause singularities. These “artificial” hot spots can adversely affect both error plots and convergence.

Crude Geometry

Point Constraints

Point Loads

As Area Zero

March 10, 2016

18 of 66

04.10 Stress Singularities

Consider the affect on error plots when a singularity is present. This situation will also cause a convergence monitor to “chase” the singularity.

To remedy this we need to either remove the singularity (e.g., with more realistic loads and/or geometry) or we need to avoid the problem areas. We can avoid problem areas/singularities by scoping convergence results.

Point Load

High Energy Gradient

March 10, 2016

19 of 66

04.11 Convergence and Scoping

A useful technique to avoid stress singularities when using convergence is to scope results away from them.

If a singularity region is not an area of interest, one can scope results to selected part(s) or surface(s) and add convergence controls only to those results.

Example:

Possible stress singularity

Region of interest

March 10, 2016

20 of 66

04.11 Convergence and Scoping

Convergence controls added to the entire model.

Geometric discontinuity causes a stress singularity causing divergence.

Solution becomes very costly by including the stress singularity.

Convergence controls on scoped results allows adaptive refinement only in user-specified locations.

Provides more control over the mesh and the adaptive solution.

Accurate stresses realized in the region of interest.

March 10, 2016

21 of 66

04.12 CAD Import

Numerous Geometry Interfaces are available for commercial CAD systems:

For the latest information on CAD geometry interfaces and supported platforms see the ANSYS Workbench Mechanical documentation.

Geometry Interface licenses can be run in reader mode for all licenses.

Geometry Interfaces can be run in plug-in mode for the CAD software listed under “Associative”.

DesignModeler is the Workbench geometry application and supports all the functions and capabilities listed for commercial CAD systems.

Note the SpaceClaim Direct modeler also supports these features.

Please note: Not all import capabilities described here are available with all CAD systems. Features depend on CAD capabilities and the support provided through the CAD vendor’s API.

March 10, 2016

22 of 66

04.12 CAD Import

Workbench geometry properties control the import of numerous CAD items in addition to geometry:

Parameters, Coordinate Systems, Material properties, etc.

To display geometry import properties:

RMB > Properties, or
View > Properties.

Geometry Interface	Availability
ACIS (.SAT)	×
AutoCAD	×
Autodesk Inventor	×
Catia V4	×
Catia V5	×
Catia V6	×
Creo Parametric	×
Design Modeler	×
Gambit	×
IGES	×
JT Reader	×
Monte Carlo N-Particle	×
NX	×
Parasolid	×
Solid Edge	×
SolidWorks	×
SpaceClaim	×
STEP	×

March 10, 2016

23 of 66

04.12 CAD Import

Import solid, surface, or line bodies:

Assemblies with mixed solids and surfaces are OK.
Select desired geometry type to filter import.
Cannot import a part with mixed solids and surfaces.

Use Associativity:

Allows updating CAD geometry in Mechanical without redefining material properties, loads, supports, etc..

Smart CAD Update:

only modified components of a CAD assembly are updated.

March 10, 2016

24 of 66

04.12 CAD Import

Local Coordinate systems:

Allows local CS from CAD models to import with geometry. See current documentation for CAD system support.

March 10, 2016

25 of 66

04.12 CAD Import

Parametric CAD dimensions can be imported into Mechanical.

Check Parameters:

The “Parameter Key” provides a filter. When used, only parameters whose names contain the key will be imported (default is “DS”).
Note, multiple filters can be used by separating each with “;” (e.g. NS; AB; VR).
To import all CAD parameters leave the parameter key field blank.

CAD parameters will appear in the Details view for the part.

March 10, 2016

26 of 66

04.12 CAD Import

Groups defined in CAD systems can be imported as Named Selections.

Check the “Named Selections” box:

The Named Selection key provides a filter. When used only groups containing the specified prefix in their name will be imported (default is “NS”).

Note, multiple filters can be used by separating each with “;” (e.g. NS; AB; VR).

To import all groups leave the named selection key field blank.
Imported Named Selections appear in the tree.

March 10, 2016

27 of 66

04.12 CAD Import

For most CAD systems Workbench offers an alternate way of working with groups of geometry via the Named Selection Manager in the CAD system.

Access the NS Manager from the ANSYS menu within the CAD system.
Once opened the NS Manager allows groups to be created independent of the internal CAD groups. Create, Select, Delete, etc. operations

Sample menu from CAD

March 10, 2016

28 of 66

04.12 CAD Import

Material Properties assigned in a CAD system can �be imported to Workbench (Engineering Data).

Check “Material Properties”:

Materials imported from CAD will appear in “Engineering Data”
Material assignments will match the CAD material assignments.

March 10, 2016

29 of 66

04.13 Defining Parameters in Workbench

Parameters are defined in Mechanical by toggling the parameter flag on/off.

Click in the square and a blue “P” will appear.
Material properties are parameterized in the engineering data application.

CAD parameters must be flagged as well to allow access in Workbench (otherwise they are read-only).

Example of input parameters

Example of output parameters

Example of CAD input parameters

March 10, 2016

30 of 66

04.14 Using the Parameter Workspace

Workbench Mechanical uses the Parameter Set workspace to manage parametric data from analysis and geometry sources.

Derived parameters and constants can be created and managed as well.

Double click or “RMB > Edit” the �“Parameter Set” to access parameters:

March 10, 2016

31 of 66

04.14 Using the Parameter Workspace

Parameter information is presented in a series of tables:

Outline: lists all input, output or derived parameters.
Property: lists information regarding the parameter highlighted in the outline.

Table of Design Points: allows multiple parameter configurations to be prepared before solving

Outline

Table of DP

Properties

March 10, 2016

32 of 66

04.14 Using the Parameter Workspace

To modify a parameter value one can enter a new value in the “Value” field in the Outline window then Update/Refresh the project.

Create custom parameters by entering expressions. Expressions can be created using functions or by using already existing parameters.

Units can be entered using braces as necessary.

March 10, 2016

33 of 66

04.14 Using the Parameter Workspace

Use the Table of Design Points to enter multiple sets values for the input parameters. This allows a number of scenarios to be predefined for study.

Once the Table of Design Points is complete, choose “Update All Design Points” to automate the solving of each scenario.

By default, each scenario overwrites the results of the previous one, retaining only the output parameter values. If you wish to retain complete results sets, check the “Retain” box for any or all rows.

March 10, 2016

34 of 66

04.14 Using the Parameter Workspace

Example using design points: A CAD dimension has been promoted to a WB input parameter.

The stress in a particular region of the model is promoted as an output parameter.
The mass of the geometry has also been promoted to a parametric output.

March 10, 2016

35 of 66

04.14 Using the Parameter Workspace

Example . . .

Opening the parameter workspace, the parameters can be seen in the outline.

In the table of design points, 3 new values are added to the current CAD parameter value.

From the top menu “Update �All Design Points” initiates the process.

March 10, 2016

36 of 66

04.14 Using the Parameter Workspace

Example . . .

The progress of the updates is reflected in the table.

With updates complete various charts can be created to investigate the data.

Stress vs Fillet Radius

March 10, 2016

37 of 66

04.14 Using the Parameter Workspace

Additional processing in the parameter workspace:

Parameter Parallel Chart shows configuration of all parameters per DP

Colored lines represent �design points.

Vertical lines represent �parameters (P1, P2, …).

DP3

DP0

DP2

DP1

Each XY intersection provides a snapshot of all parameters for a particular DP

March 10, 2016

38 of 66

04.14 Using the Parameter Workspace

By highlighting parameters, different chart configurations can be selected.

With P1 highlighted, notice that the chart options �are with respect to this parameter.

After selecting, double-click the desired chart �to configure the display.

March 10, 2016

39 of 66

04.14 Using the Parameter Workspace

As charts are created they are stored in the outline window and can be retrieved by highlighting them.

Using a RMB in various areas of the chart, �users can “Edit Properties …” to control �colors, styles, symbols, interpolation type, �legend, line display, background, etc.

March 10, 2016

40 of 66

04.15 Updating CAD Parameters

Updating from current values in the CAD tool:

After modifying the geometry in the CAD system, RMB the “Geometry” cell and “Update From CAD”. This will update the Mechanical geometry to match the CAD system.

March 10, 2016

41 of 66

04.15 Updating CAD Parameters

Updating from current values in Workbench:

Make sure CAD parameter is promoted in Mechanical.
Modify parameter value in WB Parameter Set.

Refresh: causes CAD and Mechanical geometry to match new parameter values.
Update: causes CAD and Mechanical geometry to update and remesh.

March 10, 2016

42 of 66

04.16 Workshop 04.1: Processing Results

Goal:

Analyze the mechanical arm shown below and then use some of the advanced postprocessing features to review the stress and estimate the error associated with the default mesh.

March 10, 2016

43 of 66

04.17 Workshop 04.2: Parameter Management

Goal:

Use the Workbench Parameter Workspace to setup multiple scenarios to explore structural responses in the bracket shown. Material thickness will be varied in the gusset with the bracket thickness held constant, then the process will be reversed.

March 10, 2016

44 of 66

04.18 Appendix 04.1

Additional Postprocessing

March 10, 2016

45 of 66

04.18 Appendix 04.1: Viewing Results

The Context toolbar allows for numerous alternatives for viewing results:

Vector Display Controls

Min/Max

Displacement Scaling

Display Method

Contour Settings

Outline Display

Probe

Play

Pause

Distribute

Markers

Frame Rate Control

Export AVI

Scale to Multisteps

“Timeline” allows users to animate results

Visualisation of results

March 10, 2016

46 of 66

04.18 Appendix 04.1: Viewing Results

Displacement Scaling:

In structural analysis a default scale factor “multiplies” actual displacements.
The scale factor can be changed using several built in values or to a user specified one.

True Scale

Automatic Displacement Scaling

March 10, 2016

47 of 66

04.18 Appendix 04.1: Viewing Results

We can now view results in a worksheet form.

Multiple Post-Processing entities can be viewed in one go rather than scoping individual entities under the solution branch.

RMB on solution allows users to view worksheet result summary.

March 10, 2016

48 of 66

04.18 Appendix 04.1: Legend Controls

Right Clicking on the legend in the graphics area allows the user to modify the legend display.

Edit Value

Export/Import/Switch to a saved legend setting

Horizontal/Vertical legend

Display Date/Time

Display Max/Min label on the legend

Switch to Logarithmic Scale

Switch to Scientific Notation

Number of Significant Digits

Increase/Decrease Contour Bands

March 10, 2016

49 of 66

04.18 Appendix 04.1: Legend Controls

The legend bounds can be manipulated to show result distributions more clearly for contour plots.

Click and drag contour dividers (or type in values) to specify contour ranges.

Max/Min values are unchanged

March 10, 2016

50 of 66

04.18 Appendix 04.1: Legend Controls

Independent Bands allow neutral colors to represent regions of the model above or below the specified legend limits.

Legend Contour Range

March 10, 2016

51 of 66

04.18 Appendix 04.1: Contour Controls

The “Geometry” icon controls the contour display method. Four choices are available:

“Exterior” is the default display option and is most commonly used.

“IsoSurfaces” is useful to display regions with the same contour value.

“Capped IsoSurfaces” will remove regions of the model where the contour values are above (or below) a specified value.

“Slice Planes” allow a user to ‘cut’ through the model visually. A capped slice plane is also available, as shown on the left.

Slice Planes

IsoSurfaces

Exterior

Capped IsoSurfaces

March 10, 2016

52 of 66

04.18 Appendix 04.1: Contour Controls

Capped IsoSurfaces are manipulated by an independent controller:

Icons allow isosurface cap to be top or bottom.
The cap threshold can be controlled via the slider or by typing the value directly.

Top Capped Isosurface

Bottom Capped Isosurface

March 10, 2016

53 of 66

04.18 Appendix 04.1: Contour Controls

The “Contours” icon controls the style of color bands used when plotting results:

Solid Fill

Contour Bands

Smooth Contours

Isolines

March 10, 2016

54 of 66

04.18 Appendix 04.1: Contour Controls

The “Edges” icon controls the display of the undeformed geometry or the mesh:

No Wireframe

Show Undeformed Wireframe

Show Undeformed Model

Show Elements

March 10, 2016

55 of 66

04.18 Appendix 04.1: Contour Controls

Vector plots can be used to display result quantities defined with directions such as deformation, principal stresses, and heat flux.

Activate vectors for directional quantities using the vector graphics icon:
Once the vectors are visible the vector display controls toolbar is available:

Proportional Vectors

Equal Length Vectors

Vector Length Control

Grid Aligned

Element Aligned

Line Form

Solid Form

Vector Density Control

Equal Length Vectors

Vector Length Control

Grid Aligned

Element Aligned

Line Form

Solid Form

Vector Density Control

March 10, 2016

56 of 66

04.18 Appendix 04.1: Alerts

Alerts are simple ways of check to see if a scalar result quantity satisfies a criterion:

Highlight the particular result branch, RMB and insert an Alert.
In the Details view, specify the criterion.

In the Outline tree, a green checkmark indicates that the criterion is satisfied. A red exclamation mark indicates that the criterion was not satisfied.

March 10, 2016

57 of 66

04.18 Appendix 04.1: Windows

Multiple viewports can be used to display various images at the same time (model or postprocessing data).

Useful to compare multiple results, such as results from different environments or multiple mode shapes

March 10, 2016

58 of 66

04.18 Appendix 04.1: Videos

The animation toolbar allows user to play, pause, and stop animations:

Start/Stop/Pause

Single solve results use distributed animation to interpolates results.

Export video (avi) file

Multi-solve results (e.g. nonlinear, transient) creates animation based on solution points.

Control resolution and speed

March 10, 2016

59 of 66

04.18 Appendix 04.1: Constraint Equation Display

Various operations in Mechanical result in networks of constraint equations being added to the model (e.g., remote boundary conditions, spot welds, weak springs, etc.).

Visibility for these connections is controlled from the Solution Information details and Graphics tab.

Remote Force

March 10, 2016

60 of 66

04.18 Appendix 04.1: Scoping Results

Limiting the scope of results displays can be useful when postprocessing:

Scoping automatically scales the legend to results for selected regions.

To scope contour results:

Pre-select geometry or named selection then request the result of interest.
The non-selected geometry will be displayed as translucent.

March 10, 2016

61 of 66

04.18 Appendix 04.1: Scoping Results

Results can be scoped to a single edge (or vertex):

Select edge(s) for results scoping.

March 10, 2016

62 of 66

04.18 Appendix 04.1: Scoping Results

Construction geometry consists of either a path or surface.

Paths are defined using coordinate systems, model edges or existing points.
Surfaces are located and oriented using coordinate systems.
Existing results scoped to edges can be converted to path plots automatically (RMB).

RMB

March 10, 2016

63 of 66

04.18 Appendix 04.1: Scoping Results

Results may be mapped onto construction geometry.

Path Plot Example:

Surface Plot Example:

March 10, 2016

64 of 66

04.18 Appendix 04.1: Scoping Results

Path results may also be displayed in graphical form.

The X axis may be displayed as path location (S) or time (transient analyses).

March 10, 2016

65 of 66

04.18 Appendix 04.1: Scoping Results

In addition to contoured results, a reaction probe can be scoped to a construction surface. Reactions across the surface are displayed and listed in the details.

March 10, 2016

66 of 66

04.18 Appendix 04.1: Exporting Results

To export result items, worksheet information and tables:

Highlight item, RMB > Export
For Worksheet:

Select the branch and click on the Worksheet tab.
Right-click the same branch and select “Export”.

Export as text or Excel *.xls file types.

Export Worksheet

Export Results

Export Tables

Note: To include node location information in exports, set the Include Node Location option to “Yes” under “Tools > Options … > Mechanical: Export”

March 10, 2016